yang686526

is use of a center plane for tertiary datum legit?
this may be a bit difficult to describe in words alone, but here goes.
we have a rectangular plate, on which we have designated the surface as datum feature a, the bottom edge as datum feature b. so far no problem. the width has been designated as datum feature c which establishes the mid plane of the width. now the tricky part. we/they have located 2 tooling holes with respect to primary datum feature a, secondary datum feature b, and tertiary datum feature c,(mid plane).
any thoughts or comments on the legitimacy of this callout,as relates to the tertiary of datum c specifically?
sounds legit. envisioning basic dimensions from the tooling hole c/l's to b and c/l of c with the holes perpendicularly normal to a.
if i'm getting the right visual then what you have sounds okay, as long as the datum feature identifier is shown aligned with the dimension line. if the holes are shown centered about, or on, datum plane c then no dimension is required.
powerhound, gdtp t-0419
production supervisor
inventor 2008
mastercam x2
smartcam 11.1
ssg, u.s. army
taji, iraq oif ii
ringman,
i take it you mean you applied a positional tolerance with respect to your three datums?
it sounds okay to me. your datum c is a feature of size. if this is not an accurate feature, you are going to have to do some tricky tooling, or you are going to have to call it up at mmc. is this acceptable?
jhg
the callout is legal.
just make sure that they are creating the datum reference frame correctly:
a: flat plate (3 point contact)
b: flat plate, at 90 degrees to the a plate (2 point contact)
c: two adjustable parallel plates, at 90 degrees to both the a and b plates (generally 1 point contact on each plate)
regarding legitimacy, what was the reasoning for the datum feature selection? why was it one side for b and both sides for c? one concern is that contracting the vise-like simulator for c might pull the part off of its proper 2-point contact with the b plate. the likelihood of this depends on the relative lengths of the b and c sides, and their relative squareness.

evan janeshewski
axymetrix quality engineering inc.
legit, yes. likely to be confucing to the underschooled. be prepared to do much 'splaining.
let me parrot everyone else. yes, it's good. however, if you do have concerns about it, i would suggest it is acceptable to revisit the scheme to see if alternative methods for datums exist.
matt lorono
cad engineer/ecn analyst
silicon valley, ca
ringman,
i am trying to visualize your drawing.
datum c should be applied to the width dimension. once you have done that, you can draw a centre line up the middle of your plate, and apply basic dimensions to it. forget about ± dimensions. consider doing this all some other way if the width dimension is not accurate.
jhg
sounds acceptable to me too, except i have had similar parts where i would be using the plate width as datum b (secondary) and the bottom edge as the tertiary.
so datum b is my symmetry datum and tooling holes would be in-line with the center of datum b. that way datum b can be clamped 2 points on each side for stability and the machine and/or cmm can find the center axis.
if the tooling holes were dead center, they would make a great datum b pattern datum.
ringman,
i am not able to visualise datum b since you have defined it as bottom edge, what this means are you trying to define an edge as datum ?
i agree that fundamentally it sounds legit per asme y14.5m-1994, 5.4 is an example of using pos tol wrt datum feature center planes.
is the attatched something like what you have?
i've also shown my understanding of what drawoh says about the datum feature at mmc.

kenat, probably the least qualified checker you'll ever meet...